looking for offline software for Faunc 16W controller
Close
Login to Your Account
Results 1 to 7 of 7
  1. #1
    Join Date
    Sep 2008
    Location
    Dresden, Tn
    Posts
    82
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default looking for offline software for Faunc 16W controller

    We just bought an older Fanuc Robocut with a 16W controller. This is our first EDM and we just need it for small die repair and stuff right now. I would like to be able to program it offline but it didn't come with offline software. Is there any available or do I need to look into 3rd party software? If 3rd party what is a decent inexpensive one?

    Thanks!

  2. #2
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,225
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1520

    Default

    Hi tlmkr38:
    Assuming your machine eats G code like every other Fanuc machine in creation, you have a huge variety of choices that will work.
    All you need is a post processor that will speak "Fanuc".

    I run an old old version of Mastercam Mill (version 8.1 not X8!!) and just call my cutter 0.010" diameter.
    A buddy of mine runs Bobcad and says it works fine for him too.
    Another buddy swears by Esprit, but he pays a LOT for the bragging rights and I don't think his parts are any more complicated than mine.

    Programming on a wire is not very demanding; it's setting up and processing strategy that is the big differentiator in wire work.
    Wire work is typically super accurate work and the gremlins that give you the ass bite are not usually the toolpaths...it''s the operations order and the stock allowance and the fixturing, and the stress release and the overcut allowance and the flushing and etc etc etc.

    If you're already into CNC milling, I'd first see if my milling CAM solution could be made to work.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

  3. Likes msrbl liked this post
  4. #3
    Join Date
    Aug 2002
    Location
    Regina, Canada
    Posts
    2,210
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    51

    Default

    Implex has it right on. Writing the code is the easy part. I would suggest write some real simple programs run them in dry run see how it moves. Then get some scrap put on your patience cap and try cutting. Guarantee you will run into problems you have no idea how to fix. For example, wire breaks but why? Wrong settings, bad water etc. even if you have manuals probably no help there.
    Bob

  5. #4
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    10
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    I use Cam-i and it’s quite amazing software. Just draw your part, pick your path and away you go! It’s the easiest software I have ever used for Wire EDM.
    There is a heavy cost of about $7000 for it initially but there is no yearly maintenance fees and it has every machine Fanuc build in the programming.
    I have three different wires I run and by picking the proper machine, all the tech is right there. Even taper cutting is quite easy.

  6. #5
    Join Date
    Sep 2008
    Location
    Dresden, Tn
    Posts
    82
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    All I have right now as for a 3rd party program is one called CamBam. It's inexpensive but it pretty good for what we do. I can see how programming the G code with it would work good with that on a straight cut. HOw can you use it to program like die clearance angles and stuff?

  7. #6
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,225
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1520

    Default

    Hi again tlmkr38:
    My experience with different brands of EDM machines is not very wide, but on all I have run, the most common command to run a simple non-varying taper is created by inserting a taper command word into the beginning of the code string and a taper cancel word into the end of the code string.
    On my Chmer machine which will run from the code created by a standard Fanuc post, the command to begin the taper is "A" followed by the taper angle desired (positive or negative value depending on whether you want the big end at the top or bottom of the part.
    Taper cancel is "A0".
    Every different machine brand seems to use its own unique word, so "A" may or may not work on your Fanuc.

    For the majority of taper work on punch dies this is how it's done by pretty much every machine I've seen code for.
    There is another way however, and that is to write the code for the upper profile, write the code for the lower profile and stitch them together line by line.
    This is called "Complex Upper And Lower" programming (by Sodick which was the machine on which I first learned it) and is used when the taper varies as you go around the profile.
    I am not sure if every wire machine out there can do this but I see it relatively rarely in sample code so I suspect not.

    In addition to the code, you also have to set up the machine, and this is typically done on some kind of taper setting screen in the control.

    Using my Chmer again as an example, I have a taper set screen in which I can input first of all that there will be a taper, and what it's angle will be.
    Then I can tell it how I want to instruct the machine, whether to use the "A" word, Complex Upper and Lower, or command the U and V axes directly.
    Last I can tell it how far above the platen surface I want the taper to begin...you would think of this height as the die land height if you're making punch dies.

    All of these commands are simple inputs and I believe all wires capable of cutting tapers will have a screen like this.

    On my machine it is also possible to input much of this by writing it into the code instead of commanding it from the screen, but your machine may or may not be able to do this.

    So that's really it: sounds terribly complicated but it's actually not too bad once you figure it out the first time.

    For your stated purposes, you will likely stick to the simplest way which is to manually insert the taper commands into the G code your CAM system has spit out, find and edit the values on the taper command screen, simulate the code to be sure you commanded the taper in the proper direction (Big on top or small on top as you prefer for each job), and push the big green button.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

  8. #7
    Join Date
    Sep 2008
    Location
    Dresden, Tn
    Posts
    82
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Thanks for that info. Once we get it in the room and hooked up I'm sure I'll find more of this stuff. I have all the books with the machine and it tells about how to do the manual programming and all as well as like canned cycles. Like you say once I get to using it and do more with the machine it will get easier.


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •